Incorporate new materials into the section definitions.
After creating new material definitions for each of the Simulation Composite Analysis composite materials, the next step is to incorporate these materials into the section definitions that appear in the Abaqus input file. This process simply involves changing the name of each material ply in the composite section layup to the name of a valid Simulation Composite Analysis material that was defined as described in the Define a Simulation Composite Analysis Composite Material section. For example, consider the following shell section definition from an Abaqus input file.
*SHELL SECTION, elset=PlateLayup-1, composite, orientation=Ori1, stack direction=3, layup=PlateLayup 1., 3, MATERIAL_1, 0, Ply-1 1., 3, MATERIAL_1, 45, Ply-2 1., 3, MATERIAL_1, -45, Ply-3 1., 3, MATERIAL_1, 90, Ply-4 1., 3, MATERIAL_1, 90, Ply-5 1., 3, MATERIAL_1, -45, Ply-6 1., 3, MATERIAL_1, 45, Ply-7 1., 3, MATERIAL_1, 0, Ply-8
The composite section layup contains eight material plies, where each ply is composed of a material named "MATERIAL_1". This material name should be replaced by the name of the appropriate Simulation Composite Analysis material, for example, "IM7_8552" as defined previously (Define a Simulation Composite Analysis Composite Material). The updated shell section definition is shown below.
*SHELL SECTION, elset=PlateLayup-1, composite, orientation=Ori1, stack direction=3, layup=PlateLayup, 1., 3, IM7_8552, 0, Ply-1 1., 3, IM7_8552, 45, Ply-2 1., 3, IM7_8552, -45, Ply-3 1., 3, IM7_8552, 90, Ply-4 1., 3, IM7_8552, 90, Ply-5 1., 3, IM7_8552, -45, Ply-6 1., 3, IM7_8552, 45, Ply-7 1., 3, IM7_8552, 0, Ply-8
In Abaqus/Standard only, certain elements (e.g., beam elements, shell elements, and reduced integration elements) require extraneous stiffness parameters in order to stabilize their response against deformation modes that are not governed directly by material constitutive relations. These extraneous stiffness parameters are defined as either options or data in the Section keyword statement that is referenced by the element in question. Depending upon the specific type of element being used, one or more of the following types of extraneous stiffness parameters may need to be specified as part of the Section definition that is referenced by the element.
- Section Poisson Ratio
- Section Thickness Modulus
- Section Transverse Shear Stiffnesses:
, 
, and 
- Membrane Hourglass Stiffness Control Parameter (Abaqus/Standard only)
- Bending Hourglass Stiffness Control Parameter (Abaqus/Standard only)
For any user material definition, the calculation of these extraneous stiffness parameters and their insertion in the Abaqus input file usually requires a rather cumbersome manual procedure. However, Simulation Composite Analysis includes an auxiliary program (xStiff) that automatically calculates and inserts the required extraneous stiffness parameters into the input file. The use of xStiff is highly recommended as it greatly accelerates the model building process, while at the same time minimizing the chance for errors being introduced into the input file. With the availability of xStiff, you can now postpone the task of defining the extraneous stiffness parameters until the model building process is completed and an Abaqus input file is saved. xStiff can then be run to automatically add any required extraneous stiffness parameters to the saved Abaqus input file. Please refer to the Use xStiff to Insert Extraneous Stiffness Parameters section for more information.
*COHESIVE SECTION, ELSET=Coh, MATERIAL=COHESIVE, RESPONSE=TRACTION SEPARATION, THICKNESS=SPECIFIED 1